I do not know "Sedra-Smith", but I se several problems with your circuit.

1. The current source will take forever charge a 1000F capacitor (t =C3*V/I = 1000*5/1e-6 = 5e9 seconds or about 158years. You are trying for a frequency of about 700kHz, so go to a larger current and a much smaller capacitor (0.1μF should be large enough by far).

2. L and C are unbalanced. Try multiplying L with 10 and dividing C1 and C2 by 10.

1) The biggest one were the initial conditions. After selecting "Skip the initial transient bias point calculation" (SKIPBP) in PSpice simulation's options everything got better.
2) Another big problem was in the math: I didn't size reactances well. I did it well, but just barely. In fact assuming A*B(jw0)=1 you barely get a persistent oscillation and a small rounding is enough to let it fade. So I assumed A*B(jw0)=100 when sizing reactances.
3) I had to put another small resistor in the project (R2=1f) because otherwise the simulation didn't converge, but it seems it was too small and I still had convergence problems in some circumstances. So I changed it to 1 mOhm instead.
4) The output capacitor took a long time to load (which wasn't a problem), but also lead to convergence problems in some circumstances. So I changed it to 1nF.
5) I also increased the current generator I1 to 1mA to get the oscillations sooner.
6) Finally I sized the reactances once again, assuming L=C1*10^3 to get more realistic values (but it works even if they are balanced).
7) Now THD is ~1% for the first 50 harmonics!

The reason you need a small resistance in series with the transistor base is because the (undamped) input has a small negative impedance which will tend to create a high frequency oscillation all by itself, ignoring L and C. Usually that does not create a problem in oscillators, but in amplifiers you need to watch out for those spurious oscillations.